Ansys Employee


Assuming you are selecting the face of a solid and not a surface body, the difference is that for any geometry other than a solid (face/beam edge) it will detect a direction for the bolt and split at the middle of the entity while the APDL solution runs. For a face selection, the face needs to be cylindrical type, so that it can detect an axial direction for the bolt. You may have a spline type face, rather than cylindrical if it doesn’t accept the selection. A cylindrical face type will show that in the “Selection Information” and at the bottom when you select it:

If you select a body(ies) it can’t automatically determine the direction for the bolt. That is why you need to select a coordinate system when selecting a body. It also uses the origin as the split location.

Convergence problems are an entirely different issue, and contact problems are common. But many issues can cause convergence problems, and it will be hard to diagnose such a thing in a forum without the workbench project. Is it transient or static structural? Transient can have chattering of the contact where it bounces between contact and no-contact and so uses small time step which takes a long time to run, and has convergence problems. Static analysis often has rigid body motion issue if contact is not recognized. If it converges even one subtep, you can look at a partial solution to see what’s happening. Try a very small initial time step to get a first substep convergence. If you can’t get a first subtep convergence, put a non-zero integer Newton Rhapson residual value (such as last 3 iteration residuals) in the “Solution Information” to see where problems are worst. You can also insert contact tracker under the “Solution Information” to look at number of nodes contacting and many other items. Try inserting a “Contact tool” under the Connections branch, Evaluate the “Initial information” to see if the contact is initially touching. Setting a lower contact normal stiffness factor, such as 0.1 or 0.01 often helps convergence, except where press-fit is being modeled. And try setting the “update stiffness” to “each iteratiion” or the aggressive setting. You may need to increase the pinball radius. The “adjust to touch” on the contact can help a lot for convergence if contact are meant to be in initial contact. Convergence problems can be caused by anything in the model. Geometry problems such as initial penetration of the bolt and hole body will be an issue. Mesh that is too coarse to reasonably model the curvature of the bolt is a problem too, maybe a minimum of 6 elements around the bolt shank curvature. Contacts work best with similar mesh size on contact and target sides also. Materials can also cause convergence problems although I would guess that is not the issue here.